Inventor sketch block will not delete

[william]

Hello 

I have a part file that keeps giving errors on new features, basic extrudes, etc. After digging into it, it appears to be a single sketch block & associated parameters that are the problem. 

I have tried every way i can think of to delete the parameters and the sketch block, it it refuses to be deleted. 

I have stripped the part right back to only containing the sketch block, no other parameters, sketches, or features and it still will not delete. 

I really dont want to create a new part and spend 3-4hrs rebuilding the part from scratch because of 1 sketch block. 

Can anyone figure this out? 

[johnsonshiue · Accepted solution]

Hi William,

This looks like the file is corrupted. There are still 2D sketches left in the file, even after they were all deleted. I suggest you ditch the file. Simply copy the block and paste it to a new file.

Many thanks!

[chris_graham]

@johnsonshiue, I just want to let you know that this does not seem to be an isolated file corruption issue. I have the exact same problem as @william (sketch blocks that cannot be deleted and ghost sketches that remain in the file after being deleted). This appears to be a bug related to the use of sketch blocks. If I copy one of the blocks from the original file to a new empty file, the ghost sketches appear in the new file, and the block that I just added cannot be deleted.

If you're able to investigate this bug, that would be extremely helpful; in this case, I have a very large multibody part that will take me days to rebuild, and I have no reason to believe the problem won't happen again if I continue to use blocks.

[johnsonshiue]

Hi Christopher,

Absolutely, this is a bug. Any unusual or unreasonable behavior is a bug. But, what can be done with the bug depends on the severity and if the reproducible steps exist. Were you able to reproduce the behavior?

Many thanks!

[chris_graham]

If it would help, I can post the affected file. I don't think it will be possible for me to replicate the exact steps that caused the problem. A new file with new blocks works fine; the problem didn't occur until I had been working with the file for weeks, and there's no way for me to know exactly when it started. However, the problem is reproduced in an empty part file if you copy one of the "undeletable" blocks into the file, which presumably means that the problem is related to the data of that particular block object. Hopefully you can learn something about the cause (or at least the mechanism) of the problem by looking at the data for the blocks in the part file?

As far as severity of the problem is concerned, I can't speak for other customers, but it's very severe for me. I use sketch blocks extensively for top-down design, and it's a big problem if a file that represents weeks or months of work can be corrupted for no apparent reason, forcing me to remodel it from scratch.

[johnsonshiue]

Hi Chris,

Yes, please share the file here or with me directly johnson.shiue@autodesk.com. I would like to understand the issue better.

Many thanks!

[Anonymous]

Have a similar problem, have many files that contain that block,

just deleted all items in the file and still can't delete 

Please suggest the solution 

File attached

will send the file also to the e-mail you provided

Thx, Roman

[johnsonshiue]

Hi Roman,

I suspect this is a corruption case. There was another customer reporting the same thing. He mentioned that he used multi-solid body workflows extensively. So far we are not yet able to reproduce the corruption besides the already corrupted cases.

Do you know how to reproduce it? Do you mind elaborating the typical workflow you do? At what point you found out the block cannot be deleted?

Many thanks!

[bradeneuropeArthur · Accepted solution]

This will solve it for the moment:

This is a i-logic code

Dim a As PartDocument = ThisDoc.Document

MsgBox(a.ComponentDefinition.Sketches.Count)

a.ComponentDefinition.Sketches.Item(1).Delete

[johnsonshiue]

Hi Arthur,

Many thanks for sharing the rule! I will mark it as a solution for now. However, it does not solve the underlying corruption. If you know how to reproduce it from scratch, please let me know asap. I would like to understand the workflow leading to this corruption case.

Thanks again!

[bradeneuropeArthur]

@johnsonshiue 

Strange is that if you copy the block it is also not possible to delete it!

[johnsonshiue]

Hi Arthur,

The Sketch Block folder contains the Sketch Block definitions. If there are instances of the Sketch Block in any sketch, the definition cannot be deleted. Is this what you are talking about? If not, please share an example here. I would like to take a closer look.

Many thanks!

[Anonymous]

Dear @bradeneuropeArthur, you fixed it removing a sketch that had no name, maybe it can help also here.
This the link to other thread on same topic that you solved.
https://forums.autodesk.com/t5/inventor-forum/can-t-delete-block/td-p/10525832

@william @chris_graham @Anonymous take a look!

[kimK7B54]

---

bradeneuropeArthur wrote:

This will solve it for the moment:

This is a i-logic code

Dim a As PartDocument = ThisDoc.Document

MsgBox(a.ComponentDefinition.Sketches.Count)

a.ComponentDefinition.Sketches.Item(1).Delete

---

This may be a solution, to the 2% that know how to use i-Logic.  I sure wish I was part of that 2%.  Could you give instruction on how to enter this and run it (for the other 98% of us?)

Many thanks.

[johnsonshiue]

Hi Kim,

This is pretty straight forward. Just go to the browser and enable iLogic browser -> right-click on it -> New Rule. Or, go to Manage -> iLogic -> Add Rule. After that, just copy and paste the rule here. Run the rule.

BTW, iLogic isn't just for the 2%. It is quite popular right now. It may seem overwhelming at the beginning but you will find it very easy to use. Certainly, if you want to do advanced level automation, it will require good programming skills and good understanding of Inventor API.

Many thanks!

[kimK7B54]

---

@johnsonshiue wrote:

Hi Kim,

This is pretty straight forward. Just go to the browser and enable iLogic browser -> right-click on it -> New Rule. Or, go to Manage -> iLogic -> Add Rule. After that, just copy and paste the rule here. Run the rule.

BTW, iLogic isn't just for the 2%. It is quite popular right now. It may seem overwhelming at the beginning but you will find it very easy to use. Certainly, if you want to do advanced level automation, it will require good programming skills and good understanding of Inventor API.

Many thanks!

---

Thank you;  This is more than I knew.  I hear it's popular, but still very few people know how to use it. (I've worked with about 40 inventor users, none of them knew how to use it, so 0:40 tells me less than 2% can; this is how I come up with my estimate)

Could you point me to a rescource to learn basic iLogic programming?  I've looked without success.

[johnsonshiue]

Hi! I thought my instruction was pretty clear. Anyway, here is a basic iLogic tutorial. I am not an iLogic expert either. But, I learn by using it. Please take a look. Please also help inform the 40 Inventor users about the tutorial. Hopefully, it will help them start using iLogic quickly.

https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2015/ENU/Inve...

Many thanks!

[kimK7B54]

---

@johnsonshiue wrote:

Hi! I thought my instruction was pretty clear. Anyway, here is a basic iLogic tutorial. I am not an iLogic expert either. But, I learn by using it. Please take a look. Please also help inform the 40 Inventor users about the tutorial. Hopefully, it will help them start using iLogic quickly.

https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2015/ENU/Inve...

Many thanks!

---

Your instruction was precise and it worked as far as I can tell; Thank you.  I asked for tutorial because I would like to learn how to create my own iLogic routine (I have a specific need); I do have a fear that it'll have a limitation that'll prevent it from doing what I want (after spending time learning it).  I need a program that'll automatically pull parameters from an iFeature in the .idw environment (I use iFeatures a lot).  I would like to do it within the leader command or something similar.  The current process is very tedious when I have to detail 50+ iFeatures (3+ parameters each).

Back on topic:  I ran the iLogic routine and it allowed me to delete many unwanted parameters.  There are still unconsumed parameters inventor will not purge.  Another iLogic routine perhaps?

[johnsonshiue]

Hi! If you want to retrieve iFeature dimensions in the drawing, you may simply enable "Retrieve Model Dimensions on view placement" option in Tools -> App Options -> Drawing. There is no need to create an iLogic rule for that. Is that what you were looking for?

Many thanks!

[kimK7B54]

That does not work.

This is the only dimension it brings in, and it is not a needed dimension.

I need to be able to "auto-populate" some these variables.  This would
change a 2 hour job into a 5 minute job.

Currently I have to manually find these ( in a list of up to 50
iFeatures, locate the correct one, and insert the value )

I have to go to the model to identify which iFeature I am detailing,
then back to the idw;  Very, very time consuming.